How to dimension feature patterns on drawings

Pattern Dimensioning Example
This entry is part 3 of 8 in the series Dimensions and Tolerances

A couple of days ago, I briefly covered the mythical specification “non-accumulative tolerance” (or “non-cumulative”) as it is often applied to direct dimensions on feature patterns.  See the example in Figure 1 where the dimensional callout attempts to simply dimension a pattern without considering tolerance stack-up.  However, this attempt fails since any two non-adjecent holes cannot avoid accumulation of tolerance due to the dimensioning scheme.  The problem gets worse if three or more positions within the patten are compared to each other.

Non-accumulative tolerance dimension on a pattern
Figure 1

ASME repetitive feature dimensioning scheme

ASME Y14.5-2009 actually provides a linear method to detail feature patterns, called repetitive features and dimensions.  See Figure 2. Unfortunately, the standard does not provide any tolerance rules for its prescribed scheme. Presumably, this leads us to interpret a repetitive feature dimension as though it is shorthand for chain dimensioning.  Chain dimensioning accumulates tolerance as the pattern departs from the dimensioned start position.  Sometimes this is OK, but often this is unacceptable since the accumulation of tolerance can quickly lead to features that do not align to mating features on other components.

Figure 2
Figure 2

Disorganized direct dimensions

Another dimensioning scheme that I’ve seen involves a complete disregard for the fact that a pattern exists.  See Figure 3.  Directly dimensioning each of the positions within the pattern to each other may be acceptable in some scenarios, but likely isn’t a very clear choice for larger feature patterns.  The problem with this scheme is that it can be very difficult to determine the true accumulation of the tolerance stack-up.  It may also be difficult to determine design intent.

Figure 3
Figure 3

Baseline dimension scheme

To avoid the issues associated with other direct dimensioning schemes, one may choose to use baseline dimensioning, which may also be called rectangular coordinate dimensioning in some scenarios.  The advantage of a baseline dimension scheme is that it limits the accumulation of tolerances to the stake-up from just two dimensions.  This is because the total stack-up between any two positions within the feature pattern are related through a common baseline.  The problem with baseline dimensioning is obvious in Figure 4; its take up a lot of space on the drawing.

Figure 4
Figure 4

Ordinate dimensioning

A common alternative to baseline dimensioning is ordinate dimensioning, also known as rectangular coordinate dimensioning without dimension lines.  This scheme also relies on a baseline, referred to as zero (0), from which all of the features are dimensioned.  The advantage of ordinate dimensioning is that it takes up far less space on a drawing, as shown in Figure 5.  Tolerance stack-up is limited to just two dimensions between any two positions within the pattern.

Figure 5
Figure 5

Using GD&T for best results

The best way to avoid accumulation of tolerances is to use a methodology that does not rely on any form of direct dimensions.  ASME Y14.5 actually suggests that GD&T should be used instead of direct dimensions to locate features.  I have discovered the hard way that many individuals in the engineering field have an irrational fear of GD&T.  Even still, GD&T provides a far superior method for the location of positions within a feature pattern. The example in Figure 6 shows a less cluttered drawing.  With the addition of MMC to the feature control frame, this method could provide even better results since it would make use of bonus tolerance.  The position of each feature within the pattern has an optimal tolerance zone that more closely matches design intent.  One more added benefit is that all features controlled by a single feature control frame are automatically considered as a pattern.

Using GD&T to locate features
Figure 6

Since the tolerance zone is optimized, using GD&T may help reduce costs by allowing the manufacturing process to vary in a way that is more in line with design intent.  In turn, this can reduce the number of unnecessary part rejections.


When detailing feature patterns, one may wish to avoid the use of direct dimensioning methods or shortcuts like the mythical “non-accumulative tolerance”.  The best choice to detail a feature pattern is GD&T.  However, if GD&T is not desired, the next best method is prolly an ordinate dimension scheme.  It should be noted that for each of the dimensioning and tolerancing schemes shown within this article, there are a variety of ways to implement them.  This article is meant to present general examples.  Actual tolerancing requirements are guided by design intent and other considerations per individual cases.

Author: fcsuper

As a drafter, mechanical designer and CAD engineer, I've been in the mechanical design field since 1991. For the first 8 years of my career, I was an AutoCAD professional. I utilized AutoLISP and many other AutoCAD customization features to streamline drafting activities for 6+ drafters and designers. I authored several custom functions, one of which was published in the March 1997 issue of Cadalyst Magazine. Since 1998, I've been used SolidWorks non-stop. I've worked to utilize the SolidWorks' user environment to simplify drafting and design activities for 20+ engineers. I've created this website to provide current information about SolidWorks from a variety of contributors. More recently, I am now employed by Dassault Systemes as SOLIDWORKS Sr. Product Definition Manager to improve drawing, annotation and MBD related areas.

22 thoughts on “How to dimension feature patterns on drawings”

  1. Pingback: fcsuper
  2. Pingback: Deepak Gupta
  3. I have been really happy with a combination of figure 5 (ordinate dimensions) and figure 6 (GDT with a true position callout). I prefer to have the location of each hole explicitly called out as a basic dimension. I think this makes work in the shop much easier and less prone to mistakes. SolidWorks makes this very easy with its hole table feature.

  4. merhaba solidworks
    bana gönderilen linklerin cd sini gönderirseniz sevinirim sayg?lar?mla iyi çal??malar

    Very rough translation from Turkish:
    hello solidworks
    URL links sent to you send me cd sevinirim respect? s? mla play well? studies

    I’m not sure what is being asked, but it seems like a request to download SolidWorks. If this is what is being asked, I’m not sure what avenues are available in Turkey (or whereever this request originates), but local VAR’s may have demos available. There are also student editions available.

  5. The only issue that I see here is that often times when your datums (B and C) are lined up with the dimension for the length and width, that is interpreted as the centerline of each of those dimensions being your datums.
    This means that you should indicate the start of your pattern with a dimension coming from a centerline on the part.
    Other than that, I think that this entry does a great job showing the pros and cons of each style of dimensioning patterns on a drawing.

  6. Dave, thank you for your comment. As noted, the examples in this article do not cover the full extent of possibilies. In the case of datums B and C in the last figure, it was not an accident that those are applied to the product’s centerline. It may be preferred to show a dimension back to the datum, but not absolutely necessary if the relationship between the datum and a feature is clear. My preference is to only dimension to a centerline if a feature falls along it. In part, this article is about reducing drawing clutter. The figure shows reduced clutter on a drawing without taking anything away from its meaning.

    General side note: perhaps a product does not require a centerline datum. In that case, offset the datum flag from the overall dimension. This will apply the datum one side of the part instead of its centerline. See ASME Y14.5-2009 Section 4.

  7. How would you dimension the above holes if they had 2 operations to them(ie) Top side of hole was countersunk and bottom side had a counterbore? Would you dimension just 1 hole with the mentioned operations or would you dimesnion 2 holes -each with the different operation?

  8. Drawings, by defintion in the international standards, do not normally address operations. Although holes are not assumed to be on center with one another, the dimensions to counterbores are to both the bore and counterbore. Technically, this would be treated as a separate specification for each. Tolerancing should be approached to address this. Positional tolerences offer the best method of doing so since there are specific rules that allow for better control of associated features. However, in the case of counterbores, the counterbore is usually just a clearance to house a cap screw below the part’s exterior face. As such, tolerancing is usually not a major issue. Counterbores for shoulders of two parts being slip fit together may be an example of when more consideration must be given to the counterbore’s tolerances.

  9. I have a linear hole pattern that needs a different tolerance for the first hole’s distance to the edge of the part.
    How do you use GD&T to show that?
    Let me explain it further by using your figure 6.
    Assume datum C is applied to the side of the part.
    I need the dimension .625 to have a tolerance of +/- .060 but the tolerances between the holes remain .014 and tolerances of all holes (including first) to be .014 from datum A and B.

  10. You may wish to use more than one pos tol where different limits are necessary. It may also require a different datum structure where the datums are based on the holes rather than the edges of the part. However, with knowing the design intent, it would hard to make a call.

  11. How do you properly dimension a valve stem hole in a wheel? There are no flat surfaces. What if there where more than 1 hole in the same bolt circle?

  12. There are likely several methods. I would image using a partial section view of one instance of the hole would be a start. You may have to verbosely describe the pattern.

  13. Thanks for the enlightening article fcsuper, it’s rare to see material presented in such simple clarity.

    I have a question for you. Let’s say you have a part similar to your figures above, but the holes are irregularly spaced. That is, the 9x .75 hole spacing is irregular, so even if you still use GD&T to dimension the part there will be a lot of dimensions on the page. Would you use baseline dimensioning or ordinate dimensioning if your goal is to keep the drawing visually clean? Is ordinate dimensioning acceptable per Y14.5 in this fashion?

  14. Ordinate dimensions can be used as BASIC (and, therefore, toleranced from a feature control frame). You can do this by adding the BASIC box around each of the individual ord dimensions (except your baseline 0). You can also do this by simply specifying all dimensions on the drawing are BASIC in your general notes. That way, you can still use ordinate dimensions while keeping your drawing clear and less cluttered.

  15. How would you do this dimensioning if the holes were slotted? I’m having trouble finding information online on the correct way to call out slots.

Leave a Reply

Your email address will not be published. Required fields are marked *